I'm trying to simulate a kind of mixing vessel and i have to inject a fluid inside the vessel. The problem is how to modelate or create that inlet. Is it possible to indicate to a group of nodes a mass-flow or you must have a 2d region in order to create a boundary condition?. I've created a solid inside the vessel to inject there the flow but it doesnīt work, there isn`t interaction between the vessel and the nozzle.

Thank you for reply stumpy, but could you explain a little more please?.

You advise me to create a subdomain with a continuity total source but then, i have to put a boundary condition, type inlet, in one side of the domain in order to get a flow? or it's enough with the total source?

If you add a continuity source to a subdomain, then some mass flux of fluid is introduced evenly over the entire subdomain volume. So there's no boundary condition to define, but you do have to define the properties at which the fluid is introduced (temperature, turbulence, velocity etc). If this isn't a suitable approach then yes, you do need a 2d region to define a boundary condition and it must be an external 2d region.

These days I've tried to create a subdomain with a source term but it doesn' work: i didnīt manage at injecting external flow inside the vessel. In order to overcome the problem i've created some source points which seem to work but i canīt understand the following: when i define the source point i must specify a total source mass flow (kg/s) and a velocity (m/s), so with these two values ANSYS is capable of calculate an area for that point?. Why is it necessary to give two values instead of one if it is only a point?

And i have another question. I realise when you define a boundary condition you can also specify a source term. I`ve tried to create a 2D region inside the vessel and define it as an outlet with a source term but it doesn`t work. Could you help me with the source terms, please?

Source points, boundary sources and subdomain sources are really all the same. There are all actually 3D sources. For a source point the source is introduced in the element in which the point lies. For boundary sources the elements touching the boundary are used. For subdomains all the elements in the subdomain are used. In all cases a mass flow will be needed. For the source point you provide the mass flow that is introduced in that element - so you you have introduced some mass - but at what velocity is that mass introduced? Does it just appear with no initial momentum, or is it shooting into the domain? Hence you need to specify the velocity.

Now itīs clear source points, but just the last question about this issue. If i've understood correctly you can create a subdomain, define their sides as wall boundary condition type and then include a source term in one of those sides. Thus it's possible to create a particular geometry for the nozzle inside the vessel. what do you think about this?

Those are two separate things. The only reason to create the subdomain is to add a volumetric source over the entire subdomain. If you want internal wall BC's then these would be thin surfaces, then you can add a source to those walls, but no need for a subdomain (but your geometry/mesh would need to be created with this in mind so that you have internal 2D mesh regions).

Now the idea of creating a subdomain is clear. I also understand the idea of wall BC`s as thin surfaces but what i can't really now understand, it's the following question: when you define a 2d region as an inlet you may include a source term but why?, i mean, in which case is necessary a source term instead of using a single inlet bc's?. you can create an inlet with a mixing of several materials and every material will have its own properties and initial conditions.which advantages or disadvantages have every option?.

Sorry for being a pain in the neck, but for me this issue have a lot of food for thought.